Tuesday, 7 October 2014

5 methods to get an edge aligned dimension in Inventor

It's been a long while since I last blogged, and I have really missed it. Blogging doesn't pay the bills so it takes a back seat to paying work.
Recently I had a need to place an aligned dimension between 2 holes, but whatever actions I took I couldn't get quite what I wanted. I eventually settled on rotating a Detail View and placing a standard horizontal dimension, which I can use but don't really like. I posted this to the Inventor forums and got several responses all of which are acceptable (some more than others) and I also posted this to the IdeaStation where I got further valuable input.
In this blog entry I will gather together what I have learned in the last few days about this seemingly easy requirement and the cons and pros of each method.
Method 1 - rotate a Detail View
This method is simply to create a Detail View of the area of parts you want to dimensions and then RMB on the Detail and click Rotate. Then use the rather intuitive controls to make it horizontal/vertical and then place the dimension. I finish this by adding a note to the Detail View label that the view is shown rotated. A video is posted below showing this method.
Pros - easy, placed dimension is clear, the view can be rotated again and the dimension sticks (I didn't show this in the video but it works).
Cons - not entirely intuitive to the drawing reader, requires quite a bit of work.
Method 2 - create a view sketch
This method uses a sketch on the view to create lines that the aligned dimension can be created with To start I single click the view and then select Sketch from the ribbon. Then I projected the 2 circles and the edge for dimension alignment. It's not strictly necessary to project but I do anyway. Then I created 2 connected lines, the first starting at the centre of 1 circle and the second ending at the centre of the other circle. Then I made a aligned constrain between 1 line and the projected edge I want the dimension parallel with and then a second constraint of perpendicular between the 2 sketched lines. Finally I turn 1 of the 2 sketched lines to "Sketch Only" type. I then exit the sketch and use the remaining line as the start of the dimension and the centre of the other circle as the end. A video is posted below showing this method. This method was suggested by admaiora.
Pros - relatively easy, rotation changes to the view stick.
Cons - not intuitive, requires quite a bit of work, not easily visible in the model tree.
Method 3 - chain dimension
This method uses the Chain Set dimension tools. I start by issuing the Chain Set dimension command and then select the line I want the set aligned to. Then I continue selecting the 2 holes and then RMB and select Continue to then place the dimensions. After exiting the command I then RMB on the dimension on the end and select Delete Member. I repeat this for the other unwanted dimension and am left with the dimension between the holes. A video is posted below showing this method. This method was suggested by mpatchus.
Pros - relatively easy, rotation changes to the view stick.
Cons - intuitive to regular sketch users, requires quite a bit of work, some variable results (not shown in the video but they were experienced).
Method 4 - rotated hole centre marks
This method uses the ability to rotate hole centre marks so that 1 is aligned with the direction I want the dimension at. I start by placing standard hole centre marks and then I RMB on one of then and select . A video is posted below showing this method. This method was suggested by Doug_DuPont and jletcher.
Pros - easy and intuitive.
Cons - some users/companies require centre marks to be horizontal/vertical aligned so extra commands needed to re-rotate the altered centre mark.
Method 5- centre line through tab
This method is similar to method 4. It uses a centre line through the tab near the largest hole as the basis of a dimension. A video is posted below showing this method. This method was suggested by jletcher.
Pros - easy and intuitive.
Cons - in my example this is applicable but if no tab is available or the hole is not in the middle of the tab then this method is impractical. Deleting the centre line also removes the dimension. Leaves an ugly and unwanted centre line.
Round Up
While all of the above methods have their use I feel that most miss the mark. Out of the 5 methods number 4 holds the most promise as it is intuitive, easy to implement and looks good. However I feel that there is still something missing from Inventor in relation to an aligned dimension. Thinking back to AutoCAD I could create an aligned UCS (aligned with a line) and then place the dimension and then return the UCS to world. While I'm not after this exact workflow in Inventor I feel that starting a dimension, clicking the 2 points and then a RMB and select something like Edge Align and then pick an edge is a better and even more intuitive method than that detailed in Method 4.
Feel free to make comments and suggestions. Maybe I (and the helpful forum posters) have overlooked another even better method. And many thanks to the forum posters for their help.
Footnote :- I apologise for the video window size and quality, some of which is out of my control. I'm still learning :)